Could someone assist me in finding the Q and Zeta of this Sallen Key Configuration ?

Thread Starter

Waleed El-Badry

Joined Jun 12, 2018
2
Hello,
I came by this configuration and made calculations based on Sallen-Key Equations. The cutoff filter frequency seems as usual but could someone confirm the Q-factor and Damping Coefficient equations of it? Usually, the gain resistor is conected to ground and not tied between C5 and C4.




This is the normal configuration.
 

crutschow

Joined Mar 14, 2008
24,334
Yes, that's certainly not a standard Sallen-Key configuration.
Perhaps that's an error in the schematic.
This seems likely, as the simulation below gives a very strange Bode plot:

upload_2019-6-21_0-41-55.png
 

LvW

Joined Jun 13, 2013
906
The first circuit looks - indeed - strange. However, the two series capacitors seem to indicate a highpass behaviour.
In contrast, the second circuit - called "normal configuration" - is a S&K lowpass.
So - what are you interested in?

EDIT: The simulation - as provided by chrutschow - cannot be correct.
Due to the two capacitors, the gain must start at zero (minus infinity in dB).
In fact, the circuit works as a FIRST-ORDER highpass.
The corner frequwncy (3 dB) is app. 1Hz.
 
Last edited:

danadak

Joined Mar 10, 2018
3,891
Sure looks like an integrator response approximation.

Crutschow, did you use idealized OpAmp or one with a single
pole rolloff ?


Regards, Dana.
 

ericgibbs

Joined Jan 29, 2010
9,538
hi,
This is what I see, using only 0.1Vac signal drive. [0.1Hz thru 100KHz]
E
Confirms what Carl has posted.

Filter1.PNG

Added Cartesian plot for reference.

Cart2.PNG
 
Last edited:

LvW

Joined Jun 13, 2013
906
Sure looks like an integrator response approximation.
.
I must admit that I cannot see any intergator response - neither in the circuit nor in any of the presentd simulation results.
As I have mentioned in my first answer - the circuit has a first order highpass response (created by the series capacitors).
Of course, this assumes an IDEAL opamp because it makes no sense to consider (a) a finite output impedance (which may have a considerable influence) and (b) a finite and frequency-dependent gain if we want to explain the principle behaviour of the circuit.
However, this is true for a limited frequency range only.

For very high frequencies (far above the corner of 1 Hz) the gain (which reaches a maximum of app. 40 dB) goes back to unity.
This is according to the expected behaviour of a special unity gain amplifier configuration:
The capacitors can be seen as shorts - and, thus, we have the well-known non-inverting unity gain configuration where the signal source drives the non-inv. input and at the same time the feedback voltage divider.

Evaluation of the phase response confirms this behaviour: The phase starts at -90 deg (typical 1st order highpass) and reaches -360 deg (0 deg) app. at 10 kHz (Opamp ideal).
 
Last edited:

danadak

Joined Mar 10, 2018
3,891




Sort of look similar, a little lumpy but approximate to strait line response.
G of course much lower.


Regards, Dana.
 

LvW

Joined Jun 13, 2013
906
What is the most important step during/after simulation of a circuit?
The answer: Evaluation of the results !

Applying this approach to the present task means:
Identifying the influence of unwanted/parasitic influences on the desired amplitude/phase response.

For the present case, simulation of the circuit for an ideal opamp shows that the behaviour for large frequencies (far above the highpass corner frequency of app. 1 Hz) is determined by the non-ideal properties of the used opamp model.
(There is no integration property at all - integration requires a phase shift of 90 deg.)
 

crutschow

Joined Mar 14, 2008
24,334
did you use idealized OpAmp or one with a single
pole rolloff ?
No.
The schematic shows I used an LMC6484A model.
This is what I see, using only 0.1Vac signal drive. [0.1Hz thru 100KHz]
In Spice AC analysis, linear models are used, so the magnitude of the excitation has no effect on the circuit frequency response shape, other than the displayed relative amplitude.
I use 1V excitation, since LTspice plots the dB gain relative to that level, which thus gives an absolute gain plot of the circuit in dB.
 

crutschow

Joined Mar 14, 2008
24,334
The simulation - as provided by chrutschow - cannot be correct.
Due to the two capacitors, the gain must start at zero (minus infinity in dB).
I beg to differ.
It does start at zero, but at DC, which is a frequency I cannot simulate in the AC mode (see plot below starting a 1nHz).

upload_2019-6-21_10-47-29.png
 

ericgibbs

Joined Jan 29, 2010
9,538
In Spice AC analysis, linear models are used, so the magnitude of the excitation has no effect on the circuit frequency response shape, other than the displayed relative amplitude.
I use 1V excitation, since LTspice plots the dB gain relative to that level, which thus gives an absolute gain plot of the circuit in dB.
hi,
This I know.
I chose a lower start frequency of 0.1Hz to emphasis the important lower than 1Hz response, which your original plot did not show.
I also chose a lower AC analysis signal, it is not difficult to convert to an absolute gain value, if required.
Providing the reader is made aware of the difference between our two simulations, I do not see a problem.
E
 

crutschow

Joined Mar 14, 2008
24,334
Providing the reader is made aware of the difference between our two simulations, I do not see a problem.
No problem.
I was just noting that there's generally no reason to use an excitation voltage of other than 1Vac for the AC analysis in Spice, as it does not affect the frequency response.
 

Thread Starter

Waleed El-Badry

Joined Jun 12, 2018
2
Thanks all for your assistance.

For sanity check, I made it a unity gain and it worked using the same configuration. I simulated it using two software packages giving the same cutoff as calculated. Both MultiSim and LTSpice were used

2019-06-21_19-19-54.png

2019-06-21_20-52-34.png
 

Attachments

LvW

Joined Jun 13, 2013
906
Hi Eric.....are you aware that in your circuit the 4.7 Meg is replaced by 27k ?
The peak is, of course, caused by the real opamp.
 

ericgibbs

Joined Jan 29, 2010
9,538
hi,
The TS, posted this: post #13
For sanity check, I made it a unity gain and it worked using the same configuration. I simulated it using two software packages giving the same cutoff as calculated. Both MultiSim and LTSpice were used

So I simulated his circuit.
 

LvW

Joined Jun 13, 2013
906
OK, I see. I did not recognize earlier that the TS has introduced this change.
However, as I wrote earlier - even for 4.7megOhm (and an ideal opamp model) the gain returns to unity (0 dB) for large frequencies.
 
Top